Finger Pull Profile Toolpath

[halodri]

I am testing to use a finger pull bit to cut a finger pull profile.

The Finger Pull Bit is intended to cut a finger pull profile, i.e. an undercut profile on the edge of a wooden panel.

Since the finger pull bit is quite large, I decided not to cut the profile in one path, but in 10 steps. This means I offset the final profile 10 times with a distance of 1mm. So, each offset is one mm from the next. As a result I got 10 toolpaths. This worked, but is somewhat inefficient as the router moves a lot around between toolpaths and it's a lot of work to make changes to toolpaths since there are 10 of them.

Is there an elegant way to easily combine the 10 toolpaths into a single toolpath?

I have set the bit as a 17mm downcut bit - in Vcarve - if anyone is interested I have already created a thread regarding this topic.
viewtopic.php?f=2&t=41066&p=298453#p298453

[sharkcutup]

Yup!!!

Select all toolpaths so that they are visible then this button in red in image here. Of course they all must be using same tool for this to work. Otherwise No!!!

Sharkcutup

[halodri]

Ahh , "Create Merged Toolpath". Never used that one, apparently I've got some new stuff to watch on YouTube.

Thanks for the tip @sharkcutup !

[adze_cnc]

Or… Create only one (1) toolpath. There are at least two ways to do this:

1. If you don’t mind the bit travelling from left to right then right to left, etc. Connect the ends of all the vectors so that it creates a zig-zag pattern (i.e. connect every 2nd set of lines on one end then every alternate set of lines on the other end)
2. if you need the cut to always travel in one direction then connect the end-point of each line to the starting point of the next deepest cutting line

In both cases you must tell the profile toolpath to keep the original starting point and not try to move it so that it starts outside then moves inward.

[jimwill2]

I would most likely create a "pocket" vector and run a pocket toolpath to cut out most of the material before I used the expensive bit to do the undercut. I would make it a little shallow and leave a little on the edge so the Finger Pull bit does all the finish work.

[adze_cnc]

There is a pocket toolpath in the original screen-shot so perhaps that was already thought of?

[halodri]

I would most likely create a "pocket" vector and run a pocket toolpath to cut out most of the material before I used the expensive bit to do the undercut. I would make it a little shallow and leave a little on the edge so the Finger Pull bit does all the finish work.

Hi Jim, yes this exactly what I did. First I have cut a pocket with a 8mm downcut bit that is 0.3mm shallower. I should have mentioned that.

[halodri]

Or… Create only one (1) toolpath. There are at least two ways to do this:

1. If you don’t mind the bit travelling from left to right then right to left, etc. Connect the ends of all the vectors so that it creates a zig-zag pattern (i.e. connect every 2nd set of lines on one end then every alternate set of lines on the other end)
2. if you need the cut to always travel in one direction then connect the end-point of each line to the starting point of the next deepest cutting line

In both cases you must tell the profile toolpath to keep the original starting point and not try to move it so that it starts outside then moves inward.

Your suggestion for a zigzag pattern is interesting because I tried exactly that before writing this post, but I got an error message and didn't want to troubleshot .... but now I'm encouraged to try again

[halodri]

Ok, if I try the zig zap pattern and use "Machine Vector" Outside/Right I get an error message. If I use Inside/Left it I don't get an error message but the 3D view shows something is not quite right.

I think my zigzag pattern is connected with no mistakes.

[adze_cnc]

Ah. My presumption (not having access to the file) was that with a form tool like this that you would be drawing the path so that it follows the centre of the tool and that you would be running the profiles “on the line”. Both of my suggestion will fail when set to either in or outside the line.

[sharkcutup]

Stephen (Adze_cnc)

Read the other Op's thread for the form tool Image and description. viewtopic.php?f=2&t=41066&p=298453#p298453

Sharkcutup

[halodri]

Ah. My presumption (not having access to the file) was that with a form tool like this that you would be drawing the path so that it follows the centre of the tool and that you would be running the profiles “on the line”. Both of my suggestion will fail when set to either in or outside the line.

Well, my initial offsets were set up so that the machine vectors were "outside/right". ... but ackchyually "machine vectors/on the line" works fine, I'll just adapt my line work to that..

Thank you for your help!